How to edit (device) attributes for multiple components?

[PinRudolf]

Hi,

How can I edit (device) attributes for multiple components? 

I've found that I can edit attributes using the Attribute command in the schematics, but that only works for one at a time. I've also noticed that I can batch edit using the Inspector, but that only works for Attributes I have added myself. The attributes that were part of the library are grayed out, even though they are set to variable in the device. 

I've read an eagle forum post suggestion this was an issue on MacOS but I am now running into this on Windows. 

thanks!

[PinRudolf · Accepted solution]

Ah, it does work! But you should activate the 2D PCB. It does not work from the schematic though!

Can this be reported as a bug? @jorge_garcia 

[jorge_garcia]

Hi @PinRudolf ,

I hope you're doing well. Just to clarify it works in the schematic, are you saying to make it work in the 2D PCB?

Let me know, because I'm a little confused.

Best Regards,

[craigUU3ZK]

Hi,

Not the original poster, but I am running into the same issue. In the schematic editor, if I select one or more devices and look under "Attributes" in the Inspector on the right side of the screen, all the attributes are grayed out and can't be changed.

It would be really useful to be able to select a dozen resistors to set their tolerance, for example.

[PinRudolf]

Hi Jorge,

No, sorry, it should be the other way round. It does not work in the schematic, but it does work in the 2D PCB. 

Currently, I can't batch edit attributes in the schematic when the attributes are defined by the library.

Attributes like Manufacturer, MPN or (like Craig noted) Tolerance would often be library attributes.

In the 2D PCB I can already batch edit library attributes, the problem only occures in the schematic.

Thanks

[alexandre.palardy]

Hello I get the exact same problem and yes @PinRudolf is correct. It works in the 2D PCB but not in the Schematic.

Any update on this ?

Alexandre

[robert1356]

Yes, this is a real PITA.  I put things like Dist and Dist P/N in the attributes for a part, they'll get exported on the BOM.  

I'm on MacOS, the Attribute NAMES are greyed out, but the VALUES are not. While the values don't appear greyed out, it actually allows me to double click, change the value, but then when I hit enter, the original value returns - it ACTS like it's going to change the value, but it doesn't.

Additionally, sometimes, I want to update multiples at once (like I can in a spreadsheet).  But currently, I can't see a way to do that from the schematic.  I'll try the PCB workaround.

Finally, why only change from the Attributes command.  If I select Properties of a part, it shows the attributes, why can't I change it from there.  The Attribute management needs some improvement and consistency 

[jorge_garcia]

Hi @robert1356,

I hope you're doing well. I agree this is an area that needs to be improved in Fusion 360. I'll pass these comments up the chain so that they can be addressed.

Another option in the schematic is to use the attrib-add.ulp. I've attached it for your convenience. It allows you to assign an attribute to a group of components.

Best Regards,

[DaveHolland-SET]

Hi Jorge,

Thanks for the ulp script. I tried this and I was able to add an attribute to a group of selected components placed in a schematic. It worked.

When I checked back to my libraries from where the components came - the attributes had not reflected back.

I have also tried ATTRIBUTE*  using the command line mode suggested in a post 04-18-2020 07:05 PM

(https://forums.autodesk.com/t5/fusion-360-electronics/how-to-edit-global-attributes/td-p/9453529)

This did not work and gave an error message "Use the TECHNOLOGY command to select a technology first!"

I'm really struggling with Attributes and getting them set up to be consistent in content  and useful for BOM's. I have only 10 components custom built and defined so far in my design, it's dreadfully slow and requires so many mouse clicks and movements with repetition.  Please push up the chain my message of frustration to your colleagues.

I appreciate in this role you are only a messenger.

How about helping us with another one of your helpful videos?  Titled setting up global attribute templates, say , "Part No, Unit cost, Supplier, Manufacture" as an example and apply it to all library components. 

I have spent days trying to figure this out thro trial and error and searching F360 help desk enquiries.

I see 3 years on from users posting and attributes are still not easy to use - or have I missed something?

Come on F360 team....get it fixed please.

Many thanks for your ear!

KRegards,

Dave

[jorge_garcia]

Hi @DaveHolland-SET,

So first off, attributes you define in the schematic/brd do not automatically go back to the libraries. This is by design if you are using generic parts you don't want attributes back propagating.

We are working on improving this attributes situation so the feedback is moving up the chain. In the meantime, if you want to populate a library with a default set of attributes then here's what you can do.

There is a ULP called 

run-loop-all-devicesets-script.ulp which allows you to run a script through all of the devices in the library. So all you have to do is  create a script that creates the default attributes you want. Then you can go into a library, run the ULP and feed it the script you created. That will create your default set for the entire library in one go, wether it contains 10 parts or 10000.

The global attributes are attributes that actually belong to schematic and board files and are not associated to a single component. They are used for things like design author, design version, etc.

Let me know if you have any other questions or concerns.

Best Regards,

[DaveHolland-SET]

Hi Jorge,

Thanks for a speedy response. I have had limnited success to be honest. It may be my script is too basic.

I have a test library with two components built and each has a few variants. Running my script the first time required acceptance of every new attribute, and then confirmation.  Is this normal?

On checking the attributes for each component only the head component had taken the new attributes. The variants had not. Running the scrip a second time some,  not all variants took the attributes.

One of the components is in use within a schematic. Would this cause a problem?

My script is very basic.

ATTRIBUTE M_PART_NO; ATTRIBUTE MANUFACTURER;ATTRIBUTE S_PART_NO;ATTRIBUTE SUPPLIER;ATTRIBUTE COLOUR

Any thoughts on what's going on and why the variants don't take the Attributes?

Many thanks,

Regards Dave

[jorge_garcia]

Hi Dave,

Looks like I over simplified the situation.  From the HELP page for the attribute command

First the package and technology has to be selected (in case there is more than one) and then attributes for that technology can be defined:

PACKAGE N;

TECHNOLOGY LS;

ATTRIBUTE PartNo '12345-ABC';

ATTRIBUTE Temp '100K' constant;

ATTRIBUTE Remark 'mount manually'; 

So it would seem that in order to grab all of the variants you would have to know all of the technology and package variants this information can be extracted through a ULP but I don't know if you are up for writing a ULP.

In any case, this should be much easier than it is. I'll make sure this continues to get attention.

Let me know if there's anything else I can do for you.

Best Regards, 

[DaveHolland-SET]

Hi Jorge,

I'm getting where I want to be with the libraries and Attribute sets (Technologies), Creating them and enabling them to show and being able to add my custom attributes to components and using a simple script to create multiple attribute sets to new and existing libraries.

After hours of playing, experimenting and learning, it's making more sense.

I have successfully modified and customised an imported library for LEDS (Wurth from libraryio) and taken components it through to the schematic, PCB and 3D model. So powerful.

About 160hrs in so far and still lots more to learn!

TBH it would help many newbies like me to have more detailed examples available. Please request resources from up the chain to put together.

It's a great product I must say and a big thank you to and your colleagues for  the guidance. An amazing piece of software to drive.

Thank you for your guidance and patience.

Dave

[jorge_garcia]

Hi @DaveHolland-SET,

Thanks for the feedback and the request for more documentation on device sets. I'll pass it along.

Best Regards,

[jorge_garcia]

Hey @DaveHolland-SET,

I hope this message finds you well. Could you be more specific about where more detailed examples are needed? That way our documentation team can prioritize that first.

Let me know if there's anything else I can do for you.

Best Regards,

[DaveHolland-SET]

Hi Jorge,

I'll get back to you later this week with some topic suggestions at the end of the week.

For now I'm building a couple of small simple component libraries from empty to make sure I have understood all the steps required from the schematic symbol to a rendered 3D model from a stp file using imported and my own created and modified symbols, footprints and models.

I finally worked out how to set global attributes by using the standard ULP set-all_devices_attribute and selecting my custom list of attributes and values from my script. I can now add to all my libraries my custom attributes in addition to the attributes that come with imported library.io parts. And all varients get updated.  I'm please Ihave got this far.

So yes to answer your request, I'll get a list to you of topice i belive will be useful to new users pros and hobbyists.

Dave

[DaveHolland-SET]

Hello AutoDesk team and Jorge Garcia,


I have put together some notes for you.

Hope this helps,

Dave

[jorge_garcia]

Hi @DaveHolland-SET ,

I hope you're doing well. I think you intended to attach a document but there's nothing attached.

Best Regards,

[DaveHolland-SET]

Hello Good morning.

Not Sure what went wrong...second attempt and I can see the document has
attached this time.

Dave

[pblase]

More importantly, it includes things like vendor, catalog number, and other stuff that may change between implementations. It would be very very useful to be able to change a number of properties of every component at once, preferably in a spreadsheet type setting. How about being able to read back in a BOM .csv file and back-annotate a schematic?